Tool lenght offset number is zero after each H

[fakanal]

How to fix the above mentioned problem?

See below:

N100 G00 G17 G20 G40 G49 G80 G90

T1 M06 -FACE MILL 3 INCH -

G00 G90 G55 X-2.1017 Y-5.1249 S5000 M03

G43 --> H0 <--- Z.25 M08

Z.215

 

Notice the H0 after G43!!!

It's H0 for every Tool!!

My Post is a customized 3-axis Haas Post, running

-migrated to X- on Mastercam X.

[Fred @ Slate Industries]

"If you open the control definition for that machine (from the “Machine Type” selection), and go into the TOOL section on the left of the window, make sure that “ADD to TOOL” is active and if you want the dia and length offsets to be equal to the tool number, then put zeros in the LENGTH and DIAMETER boxes and then green check out of the function saving as you exit

 

Just keep in mind that sometimes there are 2 machine/control definitions for each machine.

 

There is an MD/CD (machine Definition/Control Definition) copy that stays with Mastercam (known as the Disk or Global copy) and when you select a machine type to create a toolpath, Mastercam makes a copy of the “Disk copy” into the toolpath Manager and that one becomes the “Local Copy”

 

 

 

If you edit the MD/CD from the Toolpath manager, you are of course editing the “Local Copy” and your changes will only take effect in THAT PART FILE only.

 

If you edit the MD/CD from the “Machine Type” selection then you are editing the ‘Global Copy” and ANY OTHER part file you create with that machine type will contain your changes".

 

This fixed it for me.

The changes won't show until you start a

New Machine group in your Op.

 

HTH

[kathy]

Because of Mastercam X, the tool length offset number did not match the tool number.

 

OUCH!

 

IMO - the offset numbers should always match the tool number by default, and change ONLY when the programmer chooses to change them. Right now – in Mcam X – the numbers differ (by default / error) and I cannot find a way to reset them easily. Way back, pre version 9 I could at least double click on the tool number and all was well. So well it hasn’t been an issue until now.

 

Of course, way back when and I learned how to synchronize the tool / offset numbers, I also added a safety line to my two posts.

tlngno$=t$

So I would not have to remember to fix Mastercam all of the time.

 

This time I got bit big time using my other, more obscure post; a post where I did not add this vital piece of code.

 

The damage to the part (a very expensive part I might add) was slight, but it is damage nonetheless.

 

Tony – I experimented with your instructions and I finally got it to work. But unless CNC sees the value of a default (to the same numbers) I’m going to stick to my tried and true post override.

 

~Kathy

[Doug Gabbey]

QUOTE

IMO - the offset numbers should always match the tool number by default, and change ONLY when the programmer chooses to change them.

END

 

I COULD NOT AGREE MORE.

YES, I KNOW I AM SHOUTING.

 

DOUG

[Guest CNC Apps Guy 1]

quote:

---

...I also added a safety line to my two posts.

tlngno$=t$

So I would not have to remember to fix Mastercam all of the time.

---

AMEN!!!!!

[iowajim62]

Kathy,

 

Sorry to hear that bit of bad news.

quote:

---

This time I got bit big time using my other, more obscure post; a post where I did not add this vital piece of code.

---

I know you been doing this a long time, and as long as the spindle is ok, "all is well in the machine shop" we got more material btw, "are ya done with the 2nd one yet ?"

 

Hang in there or bail an go sailin for a day:)

[?Mark]

quote:

---

IMO - the offset numbers should always match the tool number by default, and change ONLY when the programmer chooses to change them

---

+1

Just last week scraped a part where when I copied a toolpath in op manager it didn't do a good job keeping original H offsets...

Just when I begun to trust MCX...

[?Mark]

... or MCX should at least warn me righ after I hit POST that some tool #'s and H and/or D numbers don't match...

[J Coulston]

Here is my scrap from screwy offsets.

 

[DavidB]

In the post can *tlngno$=*t$?

Or replace where it calls *tlngno$ after G43 with *t$.

 

pbld, n$, "G43", *t$, *zout, scoolant, e$

 

Would that work post gurus?

[Guest SAIPEM]

code:

---

#If Tool Length Offset does NOT equal the Tool Number

if tlngno$ < > t$,

[

#Force Tool Length Offset to match Tool Number

tlngno$ = t$

]

else,

[

#Redundant explicit assignment

tlngno$ = tlngno$

]

---

[spade117]

I don't understand why you guys are having trouble. I thought if you changed your configs to what you wanted for each tool, everything would come out ok. I haven't had any problems after I figured that out.

[gti_jay]

http://www.emastercam.com/cgi-bin/ultimate...t=019224#000000

 

I decided to add an error to my post...

 

I maintain posts for several different programmers so I don't want to "force" a certain value...

 

This way you get all the options in Mcam, but if you happen to forget...You get an error warning you.

[Charlie Pierson]

Here is the way I avoid the T-H-D mismatch problem.

Since implementing this scheme , the problem has simply gone away.

 

I use a macro-subprogram to launch every tool

In my case I tie a G code (153) to program #9013 thru parameters but

one could use G65P___ to accomplish the same task.

 

The basic idea is to copy the tool's offset to an offset register that is never used then use that

register to launch the tool.

 

ie. copy H23 to H99 then G43Z___H99 (fanuc w/ 99 offsets type C)

copy H23 to H49 then G43Z___H49 (yasnak w/ 49 offsets shared type)

 

Alter the post to output 'G153' instead of 'G43' and not output any H code

 

Sample call from main program (fanuc)

 

N20

( TOOL #5 .375 EMILL)

T22

M06

G90G55G00

G153X0.Y0.Z1.0S3800M03

(CALL TO CUTTING SUB OR CUTTING CODE HERE )

ETC.

 

Macro sub 9013 (fanuc 16m):

 

O9013(TOOL LAUNCH)

H00

G49

#111=#[#4111+2200]( SPINDLE TOOL OFFSET )

IF[#111LT2.7]GOTO9 (CHECK FOR TOOL TOO SHORT)

IF[#111LT9.75]GOTO9 (CHECK FOR TOOL TOO LONG)

#2299=#111(COPY TOOL OFFSET TO 99)

G43G00X#24Y#25Z#26S#19M#13H99( LAUNCH TOOL)

M99

N9G04P9000(STALL FOR A WHILE FOR OPERATOR TO WAKE UP)

#3000=20( CHECK TOOL OFFSET )

 

One can also do the same w/ the cutter comp offset:

#112=#[#4111+13000]( GET SPINDLE TOOL OFFSET )

#13099=#112(COPY TOOL CC OFFSET TO 99)

Then always use D99 for the CC offset.

 

cp

[kathy]

Unfortunately, we have a very expensive assembly we are machining, so an oops is just not an option. But I think the damage is minimal

I hope I hope I hope.

 

Plus, we have a green operator (very good machinist, but new to CNC) and I felt bad for him. However, for the rest of his life he will always now check the T number against the D (of H) number.

 

Otherwise, all is well –

 

Oh, except for the corner of an edge he chipped last night. I have a surface machining tool path for a transition from the top to the bottom face (gets very thin at the top) and I was using a flat diamond coated end mill. I have another diamond end mill (tapered bull nose) that we are going to use this morning.

 

~Kathy

 

And speaking of sailing – I’m going to be selling my Cal 25 this spring.

But she’s a wonderful little Delta boat, so I know I'll find a happy buyer!

[Jody]

OK for us not post smart people where do I put the code that SAIPEM posted? I am going to try it in the Start of File and Tool change Setup, after the Start of file for non-zero tool number. I will see if that is correct.

 

Jody

[Charlie Pierson]

methinks,

try inserting it just before

"pbld, n$, sg43, *tlngno$, pfzout, scoolant, pstagetool, e$" in ptlchg$ and psof$

( near the bottom of both routines )

 

cp

[Ocean Lacky™]

When I inherited the Programmer position from my predecessor, (he quit, I knew where the "On" switch on the computer was) i took the K.I.S.S. approach...4 Mills- all like tools have like Tool Numbers, ie. 1/2" ballnose is ALWAYS T3 edit the tool Library to reflect same.....I know that won't work for everyone, but it solved a lot of problems here.

[IAnderson]

So is there any way to change the defaults?

 

For instance T3 Dia offset 23 Len. Offset 4!!!!

 

Arrg @*^#*!!!!!

 

The worst part is if I change a tool in the op it resets to default. It's only a matter of time before I break somthing I have caught a bad length offset many times.

 

I use V9.1 by the way.

 

[ 04-18-2007, 05:24 AM: Message edited by: IAnderson ]

[doyleg]

i did what tony_micro did awhile back and haven't had a problem since. called my mastercam reseller about that one. i think i only lost about 3 aluminum parts.

[Bryan Johnson]

on the FTP, there is a good example of using the post to fix the problem with H and D values.

 

ftp://mastercam:[email protected]/Ma...LLX_HAAS-VF.zip